@Rik,Originally Posted by Rikk
Heres a screen shot of 4 calculators, all saying the same thing, pretty much
Simon
The material is meant to be T6 6061 ali. I know in the previous image, I t showed T4 in one of the calculators, but even after making adjustments its was still pretty close.
Cutting oil, yes, used it and applied high pressure air during the last machine run, but it still broke.
Some guides say to increase feed rate as I cant increase the rpm, surely this would apply even move sideways force to the mill?
So confused.
I used to be nervous of taking a proper cut. I've overcome this now and find that I get a much gentler action when I'm being more assertive. You have to cut slices of your material away, not scrape them off. This is why climb milling can be easier than conventional, as each tooth starts with a proper bite, rather than skidding along.
I have today run the job using a 3 flute 2mm end mill running at 5000rpm, DOC of 2 and feed of 250 as advised by the end mill provider.
This worked fantastically well without any hitches. Hooray!!
Part of this job involved some initial roughing using a 10mm 2flute with DOC of 1.7mm, rpm of 1590 and feed of 315. This also worked really well too and produced a part that I was pleased with.
So I moved on to the next part which uses the same material, 10mm end mill, DOC and feed/speeds.
This time it sounded terrible with too much vibration. Increasing the speed seemed to help, but unfortuantley, there was so much vibration one of the electrical connections to the y axis motor driver board came out!!
When I checked my 0,0 it was way out in both axis. The Y axis I can put down to MACH3 still thinking it is driving the motor, but the X being out would have to mean that the feed was too high of the speed too low, would that be a correct assumption.
Back to the drawing board on that one.
I ran another job today which required the use of my new 2mm end mills.
The first part of my tool (pocketing) using this 3fl 2mm was at 0.75mm cut depth running at 5000rpm with 250 Feed Rate, which worked ok.
The next part of the tool (pocketing) was at a 0.95mm cut depth, using same feeds and speeds, this then broke. Cutting fluid and air was used.
I have attached a couple of images to show the successful (square) and failed cut.
The mill was installed allowing about 6mm out from the collet.
If I put this data into my GWizard calculator, 2mm, 3 flute, 6mm stickout, 0.95 DOC, 5000rpm then my feed rate is coming out at 250, with an axial engagement of 47.5% well within limits.
I could drop DOC to 0.5 which would provide 25% engagement.
Not sure why this is breaking, when the conditions seem to be well within limits.
Out of interest why the change in DOC for the two jobs if they are basically the same?
Also don't forget those figures are fine in a straight line but when you get to an inside corner you have much greater engagement.
edit...no pics showing
Hi Rikk,
The reason for change of DOC is due to two different features, one having depth of 0.75 the other having 0.95 both having one plunge step.
The 0.75, square feature ran fine, even in the corners, it was the 0.95 straight line cut that caused the mill to break. A 1mm cut width was entered in to the calculator.
Attached are the missing images.
Hi Simon.
Seems like all the feeds and speeds calculators agree you're running correct feeds and speeds.
Next step is to look for other causes of breakage. Here are a few to consider:
- With small cutters, be wary of runout. I had one day in the shop where I broke 8 small 1/8" diameter EM's. Eventually I thought to check the runout and after fussing about discovered a brand new ER collet was bad. Switched collets and the problem went away. Your pictures of the cuts look awfully rough, so maybe something is going on there. If you can, measure your runout. If not, at least try different collet and chuck.
- Speaking of collets, you said you are running an ER40. That big collet takes a surprising amount of torque before you get it properly tightened. A quick hand tight on the machine won't get you there. Two hands, a reasonable amount of leverage, and a tightening fixture of some kind will get you much closer. See for example my article on using ER collets here:
Getting the Best Performance from ER Collet Chucks « « CNCCookbook CNC Blog CNCCookbook CNC Blog
You may find a smaller chuck is easier to deal with and affords more clearance as well.
- Take a look at your toolpath options in your CAM program. How are you getting the cutter into and out of the pocket? Gently helixing in is preferred, though ramping is not so bad either. Plunging is the hardest on the cutter and you'll want to make sure you use a much slower plunge feedrate. Also, I sure hope your CAM will do the initial pass at a little slower rate as it is cutting a full slot until it gets things opened up a tad.
- Take a look at a different cutting fluid. As was mentioned aluminum is sticky. Once it starts welding to the cutter the end is near. Maybe your fluid isn't providing proper lubrication? Easy way to test is turn off your fluid and try some shots of WD-40 from the can.
- Consider the aluminum itself. Some of it, especially cast aluminum, can be horrible stuff--more like taffy than metal it is so sticky. Even material certified "6061" or whatever can vary quite a bit from one source to the next. Is it possible you've just fallen into some nasty stuff? If so, chip clearance is your paramount considering. Reduce depth of cut and take more passes. Double check your chip clearing--be paranoid about any chips hanging around the cut. Last "secret weapon" for really nasty stickiest aluminum: try a single flute cutter. They sell them largely for the router crowd, but several machinists have advised me they keep some on hand for working with the worst grades of aluminum.
Hope that helps!
Best,
Bob Warfield
Try G-Wizard Machinist's Calculator for free:
http://www.cnccookbook.com/CCGWizard.html
Looking at the photo to the right, the one you see the tool breaks on, it looks like you are cutting a slot. If this is the case you maybe overloading the tool if your speed/feed calculations are based on a 1mm stepover. How is the tool entering the job, ie plunge straight in then start to feed or maybe a ramp to depth. Either way you have a stepover of more than 1mm so feeds need to be calculated to suit. A slot has a tool engagement angle (TEA) of 180deg and a straight plunge 360deg. You will need to adjust feed rates for this part of the cut.
The best way I have found for entering a cut is helical ramping as this will have a constant step over and allow for chip clearance.
Looking at the amount of burring on the edge of the cut looks like you are lacking in enough lubrication at the cutting edge causing a built up edge (material welding itself to the cutter) or a soft grade of aluminium. Be sure that the grade is guaranteed what you asked for. 6061 should be in grade t6 (hardness).
Looking at the photo of the square hole the corners are milled square so you will also get a TEA of 180deg. If your CAM program does not allow a strategy for corners (rounding, slowing the feed rate, corner peeling) you will need to program for the worst case scenario.
Gary
When you come to a fork in the road take it
are those pictures of the recent cuts using new cutters and parameters you say to be working or old pictures when you were having problems. I can tell by the buring your aluminum is clearly very soft. The 6061 that machines better is typically the artificially aged to T6 hardness 6061 which mills a lot better.
The pic on the left look almost unacceptable if done using a flat end mill. It almost looks like something with a ball nose end mill but it could be the perspective of the picture.
Likes someone said, runout could be an issue too, you should measure it with an indicator. Runout if generally consistent in the say tens of microns range, hurts smaller cutters more than larger cutters in terms of percentage. e.g. one cutting edge takes a really heavy bite than the other. If your runout is poor because the spindle is crapping out then you have to modify your milling parameters to make them less aggressive. Also, the parameters given by manufacturers or calculators are sometimes just suggestions or maximum parameters to minimize machining time. Unless the material work hardens, then the parameters are often not the 'minimum requirement' but rather the suggested or maximum you can push. You will be fine running less aggressive parameters on aluminum than the ones your calculators give you. E.g. try slowing the feed and DOC. For gummy materials you can slow down your RPM also (while maintaining feed) or alternatively increasing feed while maintaining RPM, i.e. you want the cutter to take bigger bites. But I'd definitely start with smaller DOC as the material is gummy and you may have runout issues.
@Bob
Thanks for the advise, I will be looking into runout.
Even when doing 10mm roughing/finishing I have yet to get a really decent finish, but of course there are other factors I need to consider too.
When we spoke to the Syil distributor in UK, we sent them image of the types of tools that we wanted to produce and even went and visited a local user, all said our parts were simple and should be no problem. As a complete noob to CNC, we put our trust in Syil and it was them that recommended that ER40 was the best for applications. However, knowing what I know now, ER40 is perhaps not the best solution, more so on the small end mills as we most of our work is going to be using 1.5mm drills and 1, 2, 5mm end mills. Maybe its a bit harsh, but I think we were seen coming.
For tool paths, we are just using a plunge, at the moment.
When I started looking at CAM solutions, we wanted something that would integrate into Solidworks. I tried lots of software, open source, free and subscription based too and have a spreadsheet of them all.
BobCAM are VERY aggressive on sales and dropped their price by over 50% to get the sale. In hind site, was it the best purchase? maybe not. When they did the demo, they used our supplied SW file and it looked a breeze. It wasn't a perfect demonstration in terms of click, click, click done but I wasn't expecting it to be. We used a local training BobCAD trainer, who had a very good training guide, but was just reluctant to teach based on our application. When we did get him to try, he struggled to get some tool paths to create and had no idea why. There were months of going back to him and BobCAM to get support, unfortunately, all BobCAD were interested in were trying to sell us their extended support and training.
Anyway, they finally gave in and did a live support call and even they had issues getting it too work and this just uses simple pocketing and some drilling routines.
The expectation that BobCAM could be used straight away on our part was torn apart. We now have to add a bunch of additional planes and boundary sketches to get it to create paths. Luckily for us, we built an awesome app which builds our tools in seconds based on just a couple of dimensions.
So, as it stands, we got BobCAM to produce tools paths but had to move to the next stage of making the resultant gcode work through MACH to our Syil
Reliance/assurance that the default milling parameters in BobCAM we sufficient have also taken a battering.
I appreciate that I now need to move further and perhaps choose better milling routines like spiralling to reduce stress.
I certainly learnt that trying to drill 26mm deep in this material with a 1.5mm drill bit in one pass just does not work and pecking at 2mm steps seems to work much better.
For cutting fluid, I was finding that although it appeared to be working, it was also causing chips to collect after ejecting and without a constant air supply to clear them, it was actually have a negative effect in comparison to running the same job dry (on a 10mm rough)
As for material, its a face palm moment.
The decision was made to purchase a bunch of blanks for us to use, from ChinaAlthough they are specified as T6 6061, in reality they could be anything. The old addage you get what you pay for rings true.
I have found a new single flute in a box of old bits, so I will certainly give that a go.
Appreciate your feedback.
Simon
@GazMann
Yes, you are right, the stepover is set to 50% so a 1mm and thats what the calculations have been based on. Also, the EM supplier were the ones that recommended the F&S.
I dont believe that my CAM package does have a strategy for corners, its certainly never been mentioned., but I will look into this.
Many thanks.
Simon
Why not buy some 6061 here in the UK, doesn't need to be huge chunks just enough to test out your tool paths/parameters, least then you may know if the material you have now is actually any good.
@bebob
The pictures (square pocket) are the ones that I am having issue with.
The left picture (pocket) has produced a flat pocket bottom, using a flat end mill.
More tests are definatley needed with this material and understanding our relationships with DOC etc.
The Gwizard calculator, does have an option to be aggressive, which I have wound down to be lazy.
So far from the intial cam settings we were given, machine time has increased from 45min to almost 2 hours. But hey, 2 hours is better if it works than producing crap or constantly breaking mills.
Simon
Hey Rik,
Thats next on my list, along with changing to maybe an ER20 collet system.
In fact, if we have to change to a smaller collet system and invest in a new shank ans series of collets, then we may just go for an easy change system like the Easy Change System from Coventry Toolholders.
Do you have any recommendations for ali stock sources in UK?
Many thanks.
Simon
I have a peck drilling problem (G83); while operating my Cincinnati Milacron Sabre 750 with 2100 Acrimatic controller, the code runs very well till its gets to the line where I have the G83 code and hangs the drill there, just rotating and doesn't feed in the Z-direction;
Below are the lines of codes I ran on the VMC, the G83 code went rapid to the clearance plane, then stopped there. It did not go further to drill the programmed hole (I.e it didn't feed in the Z-direction as required).
:100 T15 M6; HSS-Cobalt I (0.272inch diameter drill, 135o point angle)
N10: G0 z1.0 M08
N20: G83 X3 Y0.3189 R0Z-1.6563 K0.125 J11 F0.7 S350 M03 W1
Please any help regarding this will be appreciated.
I just buy from my local supplier W. L. Cooke Ltd not sure if they do mail order.
Just have a google lots of decent suppliers about, but as I'm just buying small/hobby amounts I've never gone further than my local.
Problem with small endmills is you need high speeds to get any kind of decent feed, do you have any images of what your making people may be able to suggest other ways of doing things.
If bobcam is that bad I'd be talking to them about some kind of refund, have to admit after reading about their products and sales technique I'd never touch them.
On the other hand I'm just about to buy sprutcam, great product and more importantly the UK distributor is a really nice guy and VERY helpful/knowledgeable.
What CNC machine do you have specifically? You mentioned syil somewhere? I dont know anything about them, but I dont think their spindles can be any more horrible than other machines. Even cheap small benchtop machines can do reasonably. Get an indicator, the type you use to square off your mill, and point the measurement at your actual cutting tool. Then rotate the tool slowly (manually if you can spin the spindle) and read off the maximum deviation. This is the runout.@Bob
Thanks for the advise, I will be looking into runout.
Even when doing 10mm roughing/finishing I have yet to get a really decent finish, but of course there are other factors I need to consider too.
When we spoke to the Syil distributor in UK, we sent them image of the types of tools that we wanted to produce and even went and visited a local user, all said our parts were simple and should be no problem. As a complete noob to CNC, we put our trust in Syil and it was them that recommended that ER40 was the best for applications. However, knowing what I know now, ER40 is perhaps not the best solution, more so on the small end mills as we most of our work is going to be using 1.5mm drills and 1, 2, 5mm end mills. Maybe its a bit harsh, but I think we were seen coming.
For tool paths, we are just using a plunge, at the moment.
When I started looking at CAM solutions, we wanted something that would integrate into Solidworks. I tried lots of software, open source, free and subscription based too and have a spreadsheet of them all.
BobCAM are VERY aggressive on sales and dropped their price by over 50% to get the sale. In hind site, was it the best purchase? maybe not. When they did the demo, they used our supplied SW file and it looked a breeze. It wasn't a perfect demonstration in terms of click, click, click done but I wasn't expecting it to be. We used a local training BobCAD trainer, who had a very good training guide, but was just reluctant to teach based on our application. When we did get him to try, he struggled to get some tool paths to create and had no idea why. There were months of going back to him and BobCAM to get support, unfortunately, all BobCAD were interested in were trying to sell us their extended support and training.
Anyway, they finally gave in and did a live support call and even they had issues getting it too work and this just uses simple pocketing and some drilling routines.
The expectation that BobCAM could be used straight away on our part was torn apart. We now have to add a bunch of additional planes and boundary sketches to get it to create paths. Luckily for us, we built an awesome app which builds our tools in seconds based on just a couple of dimensions.
So, as it stands, we got BobCAM to produce tools paths but had to move to the next stage of making the resultant gcode work through MACH to our Syil
Reliance/assurance that the default milling parameters in BobCAM we sufficient have also taken a battering.
I appreciate that I now need to move further and perhaps choose better milling routines like spiralling to reduce stress.
I certainly learnt that trying to drill 26mm deep in this material with a 1.5mm drill bit in one pass just does not work and pecking at 2mm steps seems to work much better.
For cutting fluid, I was finding that although it appeared to be working, it was also causing chips to collect after ejecting and without a constant air supply to clear them, it was actually have a negative effect in comparison to running the same job dry (on a 10mm rough)
As for material, its a face palm moment.
The decision was made to purchase a bunch of blanks for us to use, from China
I have found a new single flute in a box of old bits, so I will certainly give that a go.
Appreciate your feedback.
Simon
BobCAD cant be too bad in terms of toolpath generation. I dont use bobcad but I am sure it can do helical or ramp entry? This is better because many end mills are not center cutting, and even if they are, it is a lot easier to ramp in at an angle. Otherwise, if you are plunging, you better be going real slow. Plunging in aluminum with a 3mm end mill, 6061T6, 3000rpm, I usually do 25-30mm/s max (I recently made such a hole). Like all CAM software, there is a learning curve. The most important thing is it does the job you need it to do and this may involve learning how the software works. Its like learning a new language; mastering your mother tongue does not guarantee you will be any good at another foreign language so you will have to let go of expectations and follow the rules of the new language to succeed.
For drilling you can follow the guides. Normally you want to feed it with the correct speed so it is constantly cutting to generate continuous chip/swarf. THen you generally want to retract completely when that chip length is grown to equal to the cutting length of the drill bit.
Why not buy materials from a local source? I am sure there are metal workshops and foundries that sell material like bar stock or extrusions.
Also what do you intend to do mostly and what tools? You mentioned use of small tools. If you always plan to use small tools you may want to invest in a high speed spindle more optimized for using small tools. E.g. people doing jewelery engraving work with small end mills or engravers use high speed spindles instead. The default spindle on your mill probably cant go too high speeds and is more optimized for larger scale machining or parts using bigger end mills and say cutting steels which require slower speeds.
You need to ramp the cutter in. It's getting gummed up in your plunge.
You can try spraying wd40 on piece before plunge.
I hope this wonderful software helps. I am a metric userI am relatively new to CNC and am struggling with the whole feeds and speeds selection as I am a metric user (sorry
Last edited by axis_control; 03-20-2012 at 01:13 PM. Reason: Gramatical mistake :P
Reply with Quote
